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Phantom Piece part

BONES1369

New member
I have a fixture with the piece part assembled into it, however, the part cannot be there because then it will occur in the bill of materials. What I need is an outline of itin the drawing represented by phantom lines. Is there a way to somehow create this without the piece being in the assembly? I realize that I can just sketch the lines on the drawing, but this is very time consuming.
 
1.) Create a simplified rep. with the part excluded.


2.) Create a drawing with this rep. as the base model and insert your BOM table.


3.) Add a view using the master rep.


Unfortunately, your BOM balloons will have to reference a view without the part, and the part will show up normally in the master rep. view, but it should work...
 
You can exclude items from a BOM:



When in the drawing.



Table

Repeat Region

Filters



Pick the BOM



Filter Type

By item

Exclude



Pick the items you want excluded from the BOM.
 
or try


1. view


2. drawing display


3. component display


4. style


5. pick the part


6. select ok


7. select phantom opque or phantomtrnsp


8. done and middle mouse button
 
I regularly don't want items to list in the B.o.M. for various reasons.
For these components I set the part_number parameter to "unlisted"



and apply the filter



&asm.mbr.part_number != *unlisted*



to the table which automatically excludes all these unwanted parts. You can save and retrieve tables with pre-applied filters.



For your case you can either change the "part_number" parameter or
create a family table instance of the component with only the
"part_number" parameter changed.





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